dimensioning object from imported surface

[djwu]

Would anyone know why I can't dimension in SolidWorks? I originally created the form in Rhino, exported into IGES, and imported it into SolidWorks. Once I finished the design in SolidWorks, I created the drawing file and inserted the part files into the drawings. I tried dimensioning it without success. I went back into the part files to try to dimension the object and I can't get it to dimension most of the object. Is there anyway around this?

Thanks,
Daniel

 

[CorBlimeyLimey]

Use SW's FeatureWorks, if you have it, when you import the iges file. That will create sketches which can be dimensioned for use in the drawing.
If not, create sketches in the model, using the imported features faces & edges, then you should be able to use the sketches to place dimensions in the drawing.

from (the City of) Barrie, Ontario.

If you choke a smurf, what color does it turn?

 

[TheTick]

SW dimensions only work with points; vertices; and curves, silhouettes and edges that are linear or conic. If your imported model surfaces and edges are not planar or conic (true cylinders), you will need to do all of your dimensioning to model vertices. Set your selection filter to pick vertices and ignore edges.

Since this is imported geometry, there is a possibility that all of the surfaces are B-surfaces. If that is the case, SW will not recognize those surfaces as planar or conical, even if they appear to be so.

One way to check if a surface is planar is to attempt to place a sketch on it. Likewise, to check if a surface is conical, test it by trying to use it to create a datum axis.

There is a trick that occasionally works to convert imported B-surfaces to planes and conics. Export the model as STEP203 (not STEP214) and reimport that step file. I don't know why it works, but sometimes it just does.

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